2019 SOLIDWORKS Section View Guide [Screenshots]: Drawing, 3D viewing

What is a SOLIDWORKS Section View?

A Section View is an evaluation tool used in SolidWorks to make a temporary cut in a model for a clearer view of other areas. The section view is not limited to a planar cut and more complex sections can be extremely useful. Section views can also be imported into drawings to provide details that would otherwise be hidden from view.

The easiest way to approach the section view will first be to break down the property manager. Once we have an idea of what each of these options controls, we can approach the practical application of the “Section View” feature. To understand the options in the property manager, we’ll start at the top and work our way down…[more]

Solidworks Drawings have their own tools for producing section views, but if you’ve been using section views in a part or assembly, it can be very easy to import those views to a drawing, saving you the time of creating it twice…[more]

Abstract

As a CAD package, Solidworks offers many ways to analyze a model. One of these tools, is the section view. This tool allows a user to view a model as if a section of it were removed to give a clearer view. The cutaway is only temporary however and does not change the part or add to the feature history. While this feature is very well known, many don’t fully utilize it, and it is a much more powerful tool than most SolidWorks users realize.

How to Make a Section View in Solidworks

The idea of a section view is fairly
straightforward. As SolidWorks Help phrases it, “In a section view in a part or
assembly document, the model is displayed as if cut by planes and faces that
you specify, to show the internal construction of the model.” A simple idea but
if we take a look at the property manager for this feature, it can be very easy
to get lost in the list of options. The easiest way to approach the section
view will first be to break down the property manager. Once we have an idea of
what each of these options controls, we can approach the practical application
of the “Section View” feature. To understand the options in the property
manager, we’ll start at the top and work our way down. The first field at the
top is merely a name for our section view. The selection here is largely
preference, however, convention states that it should be a letter or pair of
letters. This comes into play a bit later. Note that this option disappears, if
you select the “Section 2” box further down the property manager. The next
selection is a choice between a planar or zonal “Section Method.” The planar
method is the easiest to understand, and works exactly as one would expect
based on the definition of a section view that was given earlier. The zonal
method, rather than just cutting by plane, cuts away a zone defined by the bounding
box of the model in question combined with the selected planes or faces. The
result is very similar with only one selection, but when multiple selections
are made, the result can be quite different. We’ll explore these differences
more when we get the the “Section 2” options a little later. The next category
is the “Section Options” area. This contains a few different options. The first
will determine how the section will calculate any offsets specified in the next
section. If we select “Selection plane” the offsets will be calculated with
respect to the plane that we selected for the section. If we select “Reference plane” then the offsets will be
calculated with respect to plane that is created by your selection, after the
application of any rotations. In general, this is one of the more obscure
options to understand, and experimenting with it is the best way to get a feel
for what will happen by changing these options. Within this same area, we also
see the “Show section cap” and the “Keep cap color” options. The first of these
will place a cap over the cut ends of solid geometry. If this is unselected,
solid geometry will appear hollow. If you have the “Show section cap” option
selected, then you may also choose to select the “Keep cap color” option. This
gives the cap that the section places over the ends of solid geometry a color
that you may select in a later option. Final we see the “Graphics-only section”
option. This option improves the speed of the resulting section but limits the
options and functionality of the resulting section. In general, unless the part
or assembly your cutting is very large, this option should be left blank. The
next area in the property manager is labeled “Section 1.” this is where we
select our first cutting plane. We can select any planar entity for this selection
or select one of the three buttons at the top of the “Section 1” area. These
buttons represent the 3 principal planes; Top, Right, and Front. Also, in this
area, you can add translations and rotations to your selected plane to
manipulate the section to the location and orientation of your choice. This
process can be repeated again in the next area labeled “Section 2,” and if
“Section 2” is selected, then a “Section 3” option will also be available.
Selecting second and third sections follows the same process as selecting the
first. However now is a good time to take a step back and mention how the
earlier option between “Planar” and “Zonal” section methods will affect how
multiple sections will cut your model. If you have “Planar” selected, the
section view will remove everything to one side of the plane. If you select
“Zonal” it changes. With “Zonal” selected, the chosen planes divide the
bounding box of the part or assembly into multiple sections, by clicking inside
the selection box beneath the “Zonal” option, you may now select one or more of
these zones to be the cut away section. This allows you to cut away complex
sections that are much smaller than would be removed with the “Planar” option.
In the next section of this article, we will demonstrate both options. The next
area of the property manager contains a selection box labeled “Section by
Body.” Note that in an assembly, this section will be labeled “Section by
Component,” but its function is identical. This allows you to select which
bodies of a multi-body part, or which components of an assembly, will be
included or excluded from the section. Once you have made one or more
selections, you can choose whether your selections are the choices to include
or exclude. The result is that the bodies that are included are sectioned,
whereas bodies that are excluded remain untouched, even if those around them
are sectioned. The next option is similar and is labeled “Transparently Section
Bodies.” Similarly, in an assembly this will be labeled “Transparently Section
Components,” but once again the function is identical. With this option,
selected bodies and components are made transparent in within the section area,
rather than being completely removed. Bodies and components excluded from this
feature will be removed as normal. As before, there are options to include or
exclude the selected bodies, and we also see a slider to determine how
transparent it makes the sections. Finally, we see an option to “Enable selection
plane.” This creates a temporary section plane that we can move around to make
selecting difficult to reach components much easier. Finally, we see the last
two options. These are buttons for “Preview” and “Save.” The preview button
merely toggles the image of the cutting plane on and off to give a clear view
of what the section will look like. The save button is a bit more interesting
and a bit more useful as well. Upon selecting the save button, we are presented
with the following menu.

If we save the view as a “View orientation” as is selected above. We can access the section again later by selecting it from the orientation dialog box as shown below.

If however we select to save our section as a
“Drawing annotation view” we get a slightly different result. Upon selecting
the new option we can see that the naming convention changes. We can still
change this to whatever we would like, but as mentioned earlier, the name of a
section usually follows the convention of being a letter or pair of letters.
The “Save As” dialog box will assume that you followed this convention and name
the view according to your selection of letter(s), repeated twice with a dash
between them as shown below.

It is worth noting here that a section view
may be simultaneously saved as a view orientation and drawing annotation view
by simply checking both boxes. Once we click save with the “Drawing annotation
view” selected, the view can be found in the annotations section of our feature
manager tree as shown below.

Double clicking this will activate our section
view. Note that if we have more than one section plane selected, section by
bodies, or transparently section bodies then we cannot save as a drawing
annotation view.

How to Create a Section View in Solidworks: Step by Step

For demonstration purposes we created a fun,
simple model that would allow us to demonstrate some of this functionality. We
start with a simple, egg-shaped model shown below.

We want to show the inside of the egg so we
start a section view.

In this model, we have created a bird cut out
inside the egg. By selecting out first plane at an angle, and our second plane
just slightly offset, we achieve a great section view for showing what’s
inside. The bird is left as a separate body, so by selecting it as an item to
exclude, we get a full view of the bird while only cutting the egg. Notice that
by selecting the “Zonal” cutting option, we can select any of the sections
created as shown here.

If we selected “Planar” for the cutting method
we would get the following result.

In this case we would stick with the zonal
method, but we want to save as a drawing annotation view, which is unavailable
with multiple planes selected. To get a similar result, we will use a single
plane at an angle as shown below, in a position that won’t touch the bird
cutout in the center.

We will save this as an annotation view called
“Section View A-A.”

Importing Section Views to Drawings

Solidworks Drawings have their own tools for
producing section views, but if you’ve been using section views in a part or
assembly, it can be very easy to import those views to a drawing, saving you
the time of creating it twice. If we create a drawing and look at the view palette,
we see that solidworks has created a “parent view” with a cutting line as well
as our desired section view.

We have to insert the parent view (in this
case the view labeled “(A) Right”) before we are allowed to insert out desired
section view. We can drag and drop those views onto the drawing one at a time
and we get the result shown below.

By default, solidworks orients our section
view normal to the cutting plane. Once we have the view inserted, however, all
we have to do is use the “3D Drawing View” tool to manipulate the view to the
orientation we want.

Conclusion

Section Views can be a powerful tool for
analysis of the model. With all the tools at our disposal, getting the exact
view we need can almost always be achieved, and if we plan ahead, we can even
use those views to annotate our drawings a little further down the line. Hopefully
you’ve the techniques we utilized here will help you get the most out of your
section views.

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Trevor Holloway is a mechanical engineer and CAD expert. He is certified in SolidWorks at the expert level (CSWE), and has years of experience in designing products for manufacture.

Trevor Holloway is driven by turning ideas into reality through engineering. He consistently seeks to push the limits of his skills and expand his knowledge base with the intent to innovate and solve problems. He enjoys viewing the engineering process holistically, from design to implementation, and always seeks to take a hands on approach. He is certified by SolidWorks as a SolidWorks Experts (CSWE).

Trevor Holloway is a mechanical engineer and CAD expert. He is certified in SolidWorks at the expert level (CSWE), and has years of experience in designing products for manufacture.
Trevor Holloway is driven by turning ideas into reality through engineering. He consistently seeks to push the limits of his skills and expand his knowledge base with the intent to innovate and solve problems. He enjoys viewing the engineering process holistically, from design to implementation, and always seeks to take a hands on approach. He is certified by SolidWorks as a SolidWorks Experts (CSWE).